[cobrakai]

Extremely helpful. Thanks Ray and tbaker.

About that 1/4" carbide end mill, thankfully I only have to go about 3/4" deep with that one. From what I've seen it actually works alright, as long as all I am doing is finishing off a few internal corners it isn't too bad. The 1.5" deep pockets require a maximum of 3/8" diameter tool though.

Okay so based on all of this information, it looks like I'll be picking up a 1/2" 2 or 3 flute roughing end mill with serrated cutting edge, and a 3/8" 3 flute high helix finishing end mill to begin. I can take 90% of the material away with the 1/2", then finish the deeper pockets with the 3/8" and the shallow pockets with the 1/4" as necessary. Seems like a logical progression.

This leads me to another question. My current end mill actually only has a 7/8" depth of cut, but I was milling 1.5" deep pockets with it. The shank ended up rubbing on the side of the pocket wall leaving a black mark, but I didn't notice any other bad effects. As long as it's just a finishing pass with minimal chips to deal with, is that acceptable practice?

Thanks again, I am amazed by the depth of help I receive on this forum!

Oh and I tried GWizard but it doesn't even let me do the trial. I'm going to try HSMadvisor.

[tbaker2500]

It's worth figuring out GWizard, email Bob if you can't get it working. It is the single most valuable tool in my tool chest.

Your plan sound good! Having the shank rub won't hurt anything. In fact, having too much cutting surface can cause problems if the tool deflects, and the whole length bites into the wall.

[cobrakai]

Since most people don't even take a full depth of cut, what's the point of having a long length of cut then? Is it just to pull the chips out of the top? I would think the stub end mills would be a lot more rigid. I'm seeing a lot of options as far as stub, regular, and extended length. I won't even go into reduced shank and whatnot.

I am now convinced that all good cnc machinists would make damn good engineers. There is so much to take into account.

[Geof]

......This leads me to another question. My current end mill actually only has a 7/8" depth of cut, but I was milling 1.5" deep pockets with it. The shank ended up rubbing on the side of the pocket wall leaving a black mark, but I didn't notice any other bad effects. As long as it's just a finishing pass with minimal chips to deal with, is that acceptable practice?

It is acceptable but not really optimal and you do run the risk of having a thin chip weld itself, or try to, into the gap between the tool shank and the workpiece and breaking the tool. I think Maritool has reduced shank end mills, I know some suppliers have them, for the very purpose of going down deep walls.

[cobrakai]

So quick update, I ended up buying a tool from MariTool. A 3/8" 3 flute carbide end mill for finishing purposes. The flutes are rather long, 1.75", so I will only be using it for taking off that last .010" on the side walls of deep pockets.

I should acknowledge that when I received the tool it had a very small nick on the tip of the cutting edge. It may or may not have affected the cutting performance and was very minor, but I mentioned it to them and they shipped me out a new one right away, no questions asked! That's great customer service.

[TiagoSantos]

I haven't read through the whole thread, but sounds like you've figured things out.. A couple months ago I was having trouble with one of my parts, it's a 3D part sculpted out of a big chunk of aluminum. I don't have flood, so I was having a lot of trouble getting through the part with decent speeds. I could slow the rpm down and make it through just fine, but any attempts to speed it up were rewarding me with chips welded to the tool and a few broken 1/2" roughers. I called the local tool place and they recommended a very expensive Iscar chatter free end mill. 1/2", high helix, carbide. It cost me almost $70 (I was in a hurry) and I was skeptical to say the least, but man does it work fantastically well. 4500rpm, 40ipm, 0.110" constant engagement at 0.6" depth of cut. No coolant, the tool stays nice and cool, the chips fly into the pan in a nice, heavy spray. The machine sounds very happy at those speeds, I could probably push it more, but it's fast enough for my purposes!

I'm sure I could achieve the same thing with a cheaper tool and eventually I'll experiment with the cheaper HSS high helix tools or even the carbide stuff from MariTool etc, but after the initial shock of paying $70 for an end mill wore off, I was very happy with the results.

[SCzEngrgGroup]

I haven't read through the whole thread, but sounds like you've figured things out.. A couple months ago I was having trouble with one of my parts, it's a 3D part sculpted out of a big chunk of aluminum. I don't have flood, so I was having a lot of trouble getting through the part with decent speeds. I could slow the rpm down and make it through just fine, but any attempts to speed it up were rewarding me with chips welded to the tool and a few broken 1/2" roughers. I called the local tool place and they recommended a very expensive Iscar chatter free end mill. 1/2", high helix, carbide. It cost me almost $70 (I was in a hurry) and I was skeptical to say the least, but man does it work fantastically well. 4500rpm, 40ipm, 0.110" constant engagement at 0.6" depth of cut. No coolant, the tool stays nice and cool, the chips fly into the pan in a nice, heavy spray. The machine sounds very happy at those speeds, I could probably push it more, but it's fast enough for my purposes!

I'm sure I could achieve the same thing with a cheaper tool and eventually I'll experiment with the cheaper HSS high helix tools or even the carbide stuff from MariTool etc, but after the initial shock of paying $70 for an end mill wore off, I was very happy with the results.

Part of your problem is no-doubt using a "rougher". That's a 4-flute tool, right? Coolant or not, 4-flutes simply don't work well in aluminum when your goal is rapid material removal. Try a 2-flute, and you'll probably be able to get much better MRR than with the rougher, perhaps even about what you're getting with that $70 tool, but for more like $12.

Regards,
Ray L.

[cobrakai]

I haven't read through the whole thread, but sounds like you've figured things out.. A couple months ago I was having trouble with one of my parts, it's a 3D part sculpted out of a big chunk of aluminum. I don't have flood, so I was having a lot of trouble getting through the part with decent speeds. I could slow the rpm down and make it through just fine, but any attempts to speed it up were rewarding me with chips welded to the tool and a few broken 1/2" roughers. I called the local tool place and they recommended a very expensive Iscar chatter free end mill. 1/2", high helix, carbide. It cost me almost $70 (I was in a hurry) and I was skeptical to say the least, but man does it work fantastically well. 4500rpm, 40ipm, 0.110" constant engagement at 0.6" depth of cut. No coolant, the tool stays nice and cool, the chips fly into the pan in a nice, heavy spray. The machine sounds very happy at those speeds, I could probably push it more, but it's fast enough for my purposes!

I'm sure I could achieve the same thing with a cheaper tool and eventually I'll experiment with the cheaper HSS high helix tools or even the carbide stuff from MariTool etc, but after the initial shock of paying $70 for an end mill wore off, I was very happy with the results.

I am curious, why are you using a rather shallow width of cut, but a rather large depth of cut? I have noticed people doing milling in multiple ways - sometimes with 60 to 80% width and maybe 20%" depth, and sometimes with 10% or 20% width and 100%-200% depth. Why would you choose either method? I can see the latter option being beneficial so you are using more of the flute length.

Is there perhaps a minimum % or minimum depth required to take advantage of a variable helix tool? This will be good to know since I also ordered a 1/2" 3 flute roughing/finishing (partially serrated flute) end mill from Lakeshorecarbide.


Also side note, I am completely blown away by this. I have constantly been using tools with a rather long length... like a 1" LOC 3/8" end mill with 1-1/2" stickout. For the first time yesterday I had to do a job that didn't require any pocketing, so I used a 3/8" 2 flute HSS end mill with only about 1/2" LOC and 3/4" stickout. The thing is so quiet and smooth, and left zero chatter marks when side milling. It really shows that you should always use the biggest, shortest tool possible.

[Steve Seebold]

Wait I'm confused. Are you saying I should trust their recommendations because they are the manufacturer and know what they're talking about, or there's a lot of marketing BS because they're trying to sell tools?

Now FYI, maybe I'm overcomplicating this for myself. Brian's talking about running 3200 pieces of something, while I on the other hand are dealing with maybe 20 or 30 of something. As such I'm only using a few tools and they will last quite a while before wearing out. Unless of course I snap them off

Tool salesman are trying to sell tou tooling based on data they have collected over the years. What they don't realize is the data they are passing to you is for applications that work great IF you have a 20 HP machine. They never have a good answer for the folks like us who only have 1.5 HP to work with.

Your salesman will tell you "oh yeah, you can make a 1/2 inch wide slot a full inch deep in one pass with his end mill. There is no effing way you're going to do that on a Tormach.

[rlockwood]

I am curious, why are you using a rather shallow width of cut, but a rather large depth of cut? I have noticed people doing milling in multiple ways - sometimes with 60 to 80% width and maybe 20%" depth, and sometimes with 10% or 20% width and 100%-200% depth. Why would you choose either method? I can see the latter option being beneficial so you are using more of the flute length.

You'll typically want to run as much axial depth of cut as limiting factors will allow (part geometry, flute length, etc) with as much radial depth of cut as the secondary limiting factors (available horsepower, part geometry, tool diameter.. etc) will allow. This isn't a golden rule, but applies pretty consistently to softer materials. Its all in playing with the variables, and learning how to make them work to your advantage.

Consider beam deflection, if you're curious why; with the additional benefit of better tool/flute utility.

[tbaker2500]

You'll typically want to run as much axial depth of cut as limiting factors will allow (part geometry, flute length, etc) with as much radial depth of cut as the secondary limiting factors (available horsepower, part geometry, tool diameter.. etc) will allow. This isn't a golden rule, but applies pretty consistently to softer materials. Its all in playing with the variables, and learning how to make them work to your advantage.

Consider beam deflection, if you're curious why; with the additional benefit of better tool/flute utility.

I would agree with this, only for external profile cuts. With that cut, you can eject the chip sideways. For internal pockets, chip removal is the dominant factor. Since pocketing usually requires some slotting, keep your Axial DOC less than 50% of the tool diameter. Otherwise, chips will pack up in the flutes to much, since they are already full from the lower part of the bit, trying to push them up the flutes, when they get packed in with the chips being cut higher up on the tool.

[rlockwood]

I would agree with this, only for external profile cuts. With that cut, you can eject the chip sideways. For internal pockets, chip removal is the dominant factor. Since pocketing usually requires some slotting, keep your Axial DOC less than 50% of the tool diameter. Otherwise, chips will pack up in the flutes to much, since they are already full from the lower part of the bit, trying to push them up the flutes, when they get packed in with the chips being cut higher up on the tool.

Eh.. i'll give you some of that, but only because we're in the tormach forum, where you're not likely to have enough surface speed and horsepower to really pull the chip out of the pocket.

In general though, as long as you are able to ramp in and create a decent sized pilot, there's plenty of room to pull the chip up and fling it well out of the pocket.

[SCzEngrgGroup]

I would agree with this, only for external profile cuts. With that cut, you can eject the chip sideways. For internal pockets, chip removal is the dominant factor. Since pocketing usually requires some slotting, keep your Axial DOC less than 50% of the tool diameter. Otherwise, chips will pack up in the flutes to much, since they are already full from the lower part of the bit, trying to push them up the flutes, when they get packed in with the chips being cut higher up on the tool.

On machines like the Tormach, with larger tools, you'll run out of spindle power long before chip removal becomes an issue, assuming appropriate tools, and correct feeds/speeds and cooling. With smaller tools, tool flex will usually limit you before chip removal does. With enough spindle power, and a high-performance endmill, you can do slotting even at depths considerably greater than the full tool diameter without chip removal problems. Chip removal typically becomes an issue more because of incorrect feeds/speeds, or inadequate coolant rather than any inherent limitation in the tool. Too high RPM or too low feed both result in reduced chipload, which is the best recipe for chip welding and clogged/broken tools, as it causes the tool to heat, rather than carrying the heat away in the chips. Of course, using the wrong tool for the job (e.g. - slotting aluminum with a 4-flute tool) is a completely different situation, and just won't work well no matter what you do.

Regards,
Ray L.

[rlockwood]

I had 1pc remaining on a nice 1.625 deep x ~3x4 pocket to run, which I thought would be an excellent example, so I broke out the camera and recorded it.. unfortunately the memory card filled up after about the first two seconds, so maybe next time. Heh..

[tbaker2500]

I will note that most of my machining is dry machining aluminum. Chip evacuation is critical. Full flood cooling gives you more leeway.

[rlockwood]

The part described was run dry, at least for the video attempt. With the parameters described, flood coolant actually impedes the chip from exiting the pocket With the disclaimer being.. It was 7075, and I wouldn't ever walk a way from the machine like that.

You're cheating yourself though.. Money spent on an enclosure and flood coolant would be much better spent than any tooling ever, especially if you're running 6061.

[SCzEngrgGroup]

...so I broke out the camera and recorded it.. unfortunately the memory card filled up after about the first two seconds, so maybe next time. Heh..

Unlucky day for digital cameras! Just made a short video of my new Novakon Pulsar doing some aggressive roughing, and when I went to zoom in, the Zoom switch *broke*, sutck in zoom-in position. Amazingly, I was able to disassemble the camera, and get it working again.

Regards,
Ray L.

[tbaker2500]

You're cheating yourself though.. Money spent on an enclosure and flood coolant would be much better spent than any tooling ever, especially if you're running 6061.

Eh, no I'm not. I've run flood for years. I hate the mess, smell, and health hazards. I moved to dry machining, and life is good. You have to get your feeds and speeds *right*, but my finishes are better than ever.

[TiagoSantos]

Part of your problem is no-doubt using a "rougher". That's a 4-flute tool, right? Coolant or not, 4-flutes simply don't work well in aluminum when your goal is rapid material removal. Try a 2-flute, and you'll probably be able to get much better MRR than with the rougher, perhaps even about what you're getting with that $70 tool, but for more like $12.

Regards,
Ray L.

Yup, you're likely right.

I am curious, why are you using a rather shallow width of cut, but a rather large depth of cut?

Others have elaborated on this better than I can, but I dunno, just seems to work better for me as far as controlling chatter. Solidcam and their constant engagement toolpaths work favorably with deeper, thinner cuts. Basically their algorithms prefer to see at least a full pitch of the helix touching the part, they say it helps reduce chatter and also uses more of the tool. I hate having endmills that are brand new and razor sharp for an inch, only to be rendered useless by a blunt or chipped tip!

[rlockwood]

I would agree with this, only for external profile cuts. With that cut, you can eject the chip sideways. For internal pockets, chip removal is the dominant factor. Since pocketing usually requires some slotting, keep your Axial DOC less than 50% of the tool diameter. Otherwise, chips will pack up in the flutes to much, since they are already full from the lower part of the bit, trying to push them up the flutes, when they get packed in with the chips being cut higher up on the tool.

I will note that most of my machining is dry machining aluminum. Chip evacuation is critical. Full flood cooling gives you more leeway.

Eh, no I'm not. I've run flood for years. I hate the mess, smell, and health hazards. I moved to dry machining, and life is good. You have to get your feeds and speeds *right*, but my finishes are better than ever.